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NX11 cylindrical dimension to baseline

Solution Partner Genius Solution Partner Genius
Solution Partner Genius

Hi,

Nx11: I have some problems with the cylindrical dimension using a baseline.

Up to Nx10 I used to place the cylindr. dimension and resize the view (Boundary, Manual rectangle) according to my need. The centerline used to remain visible (outside the newly defined boundary), and I manually hid it. The dimension remained visible.

With Nx11 the centerline is automatically hidden when the view boundary changes from automatic to manual rectangle, and my dimension also disappears. I have tried the procedure described in the Help doc (Create a single sided dimension from an invisible centerline), and it works at the beginning, but then, if for any reason you need to update the view, centerline and dimension disappear again.

I attach a movie, thanks, if anybody has suggestion.

5 REPLIES

Re: NX11 cylindrical dimension to baseline

Siemens Phenom Siemens Phenom
Siemens Phenom

Hi @Laurus,

I just checked this in NX 10 as well as NX 11 and behaviour is same as you described.

But in NX 11 it shows the information message so I guess this is the designed behaviour.centerline.PNGHowever I checked the layer settings,layer visible in view also tried to unhide/show all (Ctrl+W) objects but the diemension and centerline was not visible at all. This is unexpected for me.

 

Re: NX11 cylindrical dimension to baseline

Siemens Phenom Siemens Phenom
Siemens Phenom

@Laurus, I cheked it on solution center and found that this issue is already reported and has been converted to the PR.

NX 11.0.1 enhancement negates 'dimension from invisible centreline' method

 

Re: NX11 cylindrical dimension to baseline

Solution Partner Genius Solution Partner Genius
Solution Partner Genius

thank you very much Ganesh, you gave me a very useful hint;

I think I will add also my report of the problem to the solution center, because this problem seems to me a downgrade rather than a PR converted into ER. The suggested workflow works, but it implies that all the dimensions needed must be added once for all before re-sizing the view with manual boundary, which is very restrictive. Otherwise you have to switch back to automatic boundary and vice-versa every time you need to add a dimension (with large models is not funny...).

I also found a different workflow, that is using a sketch as a break line/detail boundary: this mantains the centerline, but again, if you need to change the boundary it is very complicate.

Re: NX11 cylindrical dimension to baseline

Siemens Phenom Siemens Phenom
Siemens Phenom
What if you were to make the section view the "Active Sketch View" and insert your own centerline (i.e., create a line, constrain it to control points and [optional] edit it's display to centerline). You can then associate your Cylindrical dimension to the sketch centerline and neither the centerline, nor the dimension, are hidden when the extents of the manual view boundary don't include the sketch centerline.

Hope that helps.
Regards, Ben

Re: NX11 cylindrical dimension to baseline

Solution Partner Genius Solution Partner Genius
Solution Partner Genius

Thank you Ben, a very good idea! Also better for me to name the sketch centerlineline, so that I can add dimensions also when the view is manually bounded and the sketch centerline is not visible.